## Quick Overview

This Tips & Trick shows how to use an Simcenter 3D formula field and face’s isolines to easily define a spatially-varying pressure load.

*Figure 1. Spatially-varying pressure load*

## Core content

Let’s assume that it is intended to define a pressure distribution over the face shown in Figure 2, such that the maximum pressure occurs at the center of the geometry and gradually decreases to zero at the edges.

*Figure 2. Arbitrary geometry*

A simple way of defining such a load distribution on an arbitrary face is with the face’s ISO lines. In Simcenter 3D, it is only required to define the extreme ISO lines, i.e. U=0, U=1, V=0, and V=1, and NX will automatically create the intermediate lines. Figure 2 shows the extreme values for the ISO lines on the face. Note that U and V definitions are interchangeable.

*Figure 3: ISO lines for the arbitrary face*

The next step is to define a function in terms of U and V that satisfies the requirement of maximum value at the center, i.e. U=0.5, V=0.5, and zero values at the edges, i.e. U=0, U=1, V=0, and V=1. There are many functions that can define such a distribution, a simple one would be:

P(U,V)=P0*sin(180*U)*sin(180*V)

Where P0 is the magnitude of the pressure at the center, which is assumed to be 1 in this example.

## Steps

In the sim navigator, define a new load as **nodal pressure**. Under the **Model Object** group, select the face on which the load is to be applied, and then in the **Magnitude **group choose New field->Formula.

*Figure 4. Defining a Formula Field*

In the Formula Field dialog, under the Domain group, select the independent variable to be **Parameter Plane**. Then in the Spatial Map group set the type as **Parametric Plane** and set the Mapping as **ISO Lines**. You may need to expand **Spatial Map** section.

*Figure 5. Defining the Isolines*

Under the **ISO Lines (u)** and **ISO Lines (v)** groups, select the edges that define U and V as shown in Figure 2. Note that after selection of the edge(s) that define either of ISO lines, it is required to click the **Add New Set** before proceeding to the definition of the next ISO lines.

Then under the **Expressions **group, enter the function that defines the pressure distribution and click OK.

*Figure 6. Defining the pressure load expression*

To graphically verify the load distribution, in sim navigator, right click on the defined load and select **Plot Contours**.

*Figure 7. Make a contour plot of the applied load*

Then, a contour plot of the applied load will be generated in Simcenter 3D.

*Figure 8. Spatially-varying pressure load*